How to define the Reynolds Number in CFX?
Hi, I just find a problem by using CFX. In my case of flow around a circular cylinder, the Reynolds number was defined by the reference value which was named global length not the diameter of the cylinder. What is the global length? And how to define the Reynolds number by the relevant parameters in CFX?
Thanks a lot ! Y.F.Lin 
Re: How to define the Reynolds Number in CFX?
Hi,
I suppose you're talking about the Reynolds Number and the Global Length values present in the .out file. The Global Length is simply the cubic root of the volume, and this Reynolds number is merelly an indicative value. CFX doesn't know what is your characteristic length. I'm sure you don't need a CFD software to calculate the Reynolds number, actually you should calculate it before doing anything with the software. But if for some reason you want to obtain it in CFX, create an expression Re=Rho*U*L/niu Regards, Rui 
Re: How to define the Reynolds Number in CFX?
Ok, I understand it.
Thank you very much. yflin 
low Reynolds number
Hi,
I'm simulating flow over microroughness and getting very low Re<<1 (as my domain size very small and velocity also). Can anyone suggest how to put exact value of Re (e.g. 100,200) in ANSYS CFX_13? How can I get characteristic lengh, L value if I want to put in Re equation? R Partha 
Do you want to run a simulation at a specific Re number or do you want local Re numbers reported in a flow?

Hi,
I want to run a simulation at a specific Re number (e.g. 100,200,250). the fluid domain I choose 230*70*15 micrometer^3 only and rough (e.g. riblet,semicircular) at bottom only. as given fluid velocity at top 0.0002 m/s (like Couette flow) with pure water, I got local Re<<1. So I wanted to check the simulation with specific Re number. Could you suggest if my existing model Ok or not? I found very low Re turbulence and it does not cover any turbulence model Re range. So is the flow purely laminar? I took a very zoom in view of a turbulent flow near to the wall within viscous sublayer and applied microroughness there. I wanted to find out how roughness destroys laminar zone close to wall. Pls give some idea if I should go with specific Re, and if so how can I get it in CFX? Thanks for your reply. Partha 
Quote:
What definition of Re number do you mean for running at 100, 200, 250? What is your length and velocity scales? 
Quote:
let me explain my situation. I'm modeling a part of fully developed turbulent flow which is very near to the wall. And this region is highly viscous dominated laminar/creeping flow as you mentioned. I didn't take the whole fluid domain but the very surface near zone as mentioned in the work by (Friedmann E. 2010. The Optimal Shape of Riblets in the Viscous Sublayer. J math fluid mech 12:243265) Should I increase domain size and velocity for getting Re~1 or more instead of Re~1e5, or should I go for specific Re value with v*D/neu eqn? D=wetted perimeter or length scale, v=free stream velocity. In some literature, people used specific Re value for microfluidic analysis. I dont know how they define it. Is it possible to define Re so specifically in CFX with any measurement? R Partha 
You can make the domain any size you like. It just needs to be big enough to containt he features you want to study, plus the normal sensitivity check of boundary proximity. For this condition you can apply an inlet boundary which matches the laminar flow gradient as you move away from the wall.
Three big problems you are going to have to contend with: 1) The CFX residual calculation does not work very well at very low Re number. You are going to have to do a careful sensitivity analysis to find appropriate convergence levels. The general guide of 1e4 for a start and 1e5 for an accurate solution will nto apply. 2) The pressure gradient is not normal to the wall at very low Re. It holds only for high Re number flows. I suspect CFX has normal pressure gradients at walls hardcoded into it (but I have not checked). If this is the case then CFX will give you a big error. 3) Likewise, the usualy exit boundary condition is a pressure boundary. Unless you can analytically derived the pressure field as you travel away from the wall your exit boundary will be wrong. You can get around this by simply moving your exit boundary far enough down stream that it does not affect the area of interest. I suspect point 2 might be a showstopper for CFX. Unless you can confirm that CFX correctly applies the pressure BC at a wall then you will have to find another code which will do it. 
Thanks a lot for your explanation and guidelines..it would help me a lot. I would like to keep communication in future also.
Thanks again. R Partha 
Reynolds number
Hi All
I want to define a new drag model then I need to define Reynolds number that is a function of my particles velocity. My problem is in CFXPre I can't find a way to correlate Reynolds based on changing velocity, I have to put initial velocity of particles (that is constant) this would affect my drag model. Thank's Sep 
I do not understand your question. Are you having problems calculating the particle Re number? Are problems implementing you drag law?

Hi ghorrocks!
Since you have said me to read this post, I will write here my question. I have read the questions and the relative answers but I did not find the solution for my problem. I have a 2D problem. I created the mesh with ICEM and then I extruded it with the shrewdness of to put as depth, 1 cell like thikness. After importing the mesh in CFX, I have put boundary condition of symmetry for to simulate the 2D problem. I have these measures of the rectangular channel: Length: 3900 mm Heigth: 50 mm (Characteristic length L) Depth: 1 cell like thikness Re= 80000 (known input of the problem) Velocity along x axis= 24 m/s (u) at the inlet. The other velocities are 0 m/s. No swirl component. Dynamic viscosity: 1.8058e05 kg/m*s (alpha) Density: 1.20438 kg/m^3 (beta) Kinematic viscosity: alpha/beta= 1.4993e5 (ni) Re= (u*L)/ni ~ 80000 [for precision 80034] But Ansys has given me Re=9.2723E+04 How can I do for to solve this problem? Thanks 
CFX doesnt know your characteristic length, so it assumes L = domainvolume^(1/3). Thus, the Reynolds number given by CFX is just an estimation, and nothing else. It never uses the Reynolds number in the calculation.

Quote:
Also ghorrock has said me this. So, I must trust of my known inputs and to neglect Ansys' results. Ok! If I can leave my displeasure, here Ansys with his fictional Re number leaves me perplexed. 
The purpose of the Re number reported is just a general guide for the flow, in particular to have a guess as to whether a turbulence model should be used. If it says the Re is high and a laminar flow model is being used it shows a warning saying maybe you should use a turbulence model. That is all the Re calculation does.

Ok... I thought that Re has influenced also the turbolent model!
Thanks 
Hi everyone
Has anyone checked the velocity that CFX gives in the "Average Scale Information"???? Actually I have made 2 geometries kind of the same with a tiny difference in their thickness. It is made of 3 pipes(one as the inlet pipe bringing the fluid into a big tank and the other 2 pipes let the fluid goes out). the difference is between the thickness of the big tank in these 2 geometries and all other measurements like the inlet velocity, outlet pressure(0) and the dimensions are the same. when I run the CFX solver, I got different Reynolds number ~80 for one and 3.4E+4 for the other one. As I have checked, what is different among these 2 in the CFX solver is in the "Average Scale Information" > Global Length, velocity and the Advection time. I can calculate the Global Length as the Ansys do. But my problem is with the Advection time and consequently the velocity that makes my Reynold's number so big!! Can anyone help me? I appreciate the time you put to read and answer my question. I really could use your experience and knowledge to find out my problem. Thank you so much Rojan 
Did you read my post #16? The reported Re is not used for anything in the calculation and is just used to generate a warning message about turbulence if a laminar flow is modelled. And it is just a warning which you can ignore if you know is it OK. So ignore it

Thank you for your response
yes I read it and I ignored it and let the program run. It seems that just the stream line are so messy and turbulent. Basically the streamlines of these two geometries are completely different! As I checked other stuff, all of them are kind of the same for both. May I ignore the streamlines too!!? Thanks again. Rojan 
All times are GMT 4. The time now is 07:09. 